CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Formulation in compressibleInterFoam

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree33Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 20, 2019, 06:36
Default
  #61
Senior Member
 
Daniel
Join Date: Mar 2013
Location: Noshahr, Iran
Posts: 348
Rep Power: 21
Daniel_Khazaei will become famous soon enough
Quote:
Originally Posted by dduque View Post
Just a quick note to this, dduque, is my usual name. I had to use the previous one, ddcampayo, due to some glitch in the CFD-online user management system.

BTW, I am quite convinced my interpretation is mostly correct, with some technical details that I had wrong. If anyone is interested I can correct those.
Hi,

Well I'm interested
Would you please share your findings?

I'm trying to do the exact same thing.

Regards
EngMec likes this.
Daniel_Khazaei is offline   Reply With Quote

Old   April 17, 2020, 08:49
Default Energy equation
  #62
New Member
 
saeedbd
Join Date: Feb 2015
Posts: 6
Rep Power: 11
saeedbd is on a distinguished road
Hi foamers,

I am working on CompressibleInterFoam. I want to convert the T equation to a general energy conservation equation to remove some assumptions in the solver. Could you finally manage the energy equation?

Assuming the perfectGas and perfectFluid Eos, we have e=Cv*T for each phase where e is internal energy. So, I am replacing T with et/(Cv_water Y_water + Cv_air Y_air) in the solver (et is the total internal energy with et = e1*Y1 + e2*Y2. But it gives me wrong results for bubble collapse case. So in fact, the T equation in original solver is as:

Code:
fvScalarMatrix TEqn                                                                 
    (                                                                                   
        fvm::ddt(rho, T) + fvm::div(rhoPhi, T) - fvm::Sp(contErr, T)                    
      - fvm::laplacian(turbulence.alphaEff(), T)                                        
      + (                                                                               
            fvc::div(fvc::absolute(phi, U), p)()() // - contErr/rho*p                   
          + (fvc::ddt(rho, K) + fvc::div(rhoPhi, K))()() - contErr*K                    
        )                                                                               
       *(                                                                               
           alpha1()/mixture.thermo1().Cv()()                                            
         + alpha2()/mixture.thermo2().Cv()()                                            
        )                                                                               
     ==                                                                                 
        fvOptions(rho, T)                                                               
    );

and now is converted to

Code:
fvm::ddt(rho, et) + fvm::div(rhoPhi, et) - fvm::Sp(contErr, et)
      - fvm::laplacian(turbulence.alphaEff(), et)
      + (
            fvc::div(fvc::absolute(phi, U), p)()()
           // - contErr/rho*p 
          + (fvc::ddt(rho, K) + fvc::div(rhoPhi, K))()() - contErr*K
        )
      *(
           alpha1()/mixture.thermo1().Cv()() + alpha2()/mixture.thermo2().Cv()()
       )
      *(
         Y1*mixture.thermo1().Cv()()+Y2*mixture.thermo2().Cv()()                        
         )
        ==
        fvOptions(rho, et)


where Y is the mass fraction: et=Y1*e1 + Y2*e2 and e1=Cv1*T , e2=Cv2*T.


Also, I tried:

Code:
fvm::ddt(rho, et) + fvm::div(rhoPhi, et) - fvm::Sp(contErr, et)
      - fvm::laplacian(turbulence.alphaEff(), et)
      + (
            fvc::div(fvc::absolute(phi, U), p)()()
           // - contErr/rho*p 
          + (fvc::ddt(rho, K) + fvc::div(rhoPhi, K))()() - contErr*K
        )
        ==
        fvOptions(rho, et)


But it does not work properly as well. The temperature drops at the interface immediately. In more details, I don't know why et in the new energy equation remains constant while I checked that we have velocity and K is NOT zero! (How can it be possible?) Then, after a very small time step 10^-12, since we have Y_water = 0.1 in the gas side of the interface, Temperature drops suddenly according to T = et/(Cv_water*Y_water + Cv_air*Y_air).

The last point, it gives good results for the shock tube case which is not very dependent on temperature and energy.

Do you know how to solve the issue? Thank you for your time.

Saeed,
saeedbd is offline   Reply With Quote

Old   April 17, 2020, 13:19
Default
  #63
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi,


so I am not familiar with the solver you are using and I am also not familiar with its equation. However, VOF solves only one question for energy/momentum and so on. Just one question, you are solving for the field et, which is what? An energy right, the total internal energy. So, how do you transform the energy back into the temperature? I cannot see anything here. Because, as you are not solving for T anymore, the T field should stay constant.

So actually, what you have to do is:
  • If possible, introduce a energy equation (maybe the one you have is fine)
  • Furthermore, you need to have the transformation from T -> e and back from e -> T


Hope this might help.
Tobi
saeedbd likes this.
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   April 17, 2020, 13:44
Default
  #64
New Member
 
saeedbd
Join Date: Feb 2015
Posts: 6
Rep Power: 11
saeedbd is on a distinguished road
Hi Tobi,

Thank you very much for giving your feedback. Regarding the Temperature, I am obtaining it within the T = et/(Cv_water*Y_water + Cv_air*Y_air) equation which is based on perfectFluid and perfectGas. So to put it into a nutshell, I initialize the system with et=e1Y1+e2*Y2 and then solve the et equation. Then I update the T, based on the new et using the above equation.

Best,
saeedbd is offline   Reply With Quote

Old   April 17, 2020, 14:31
Default
  #65
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51
Tobi has a spectacular aura aboutTobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Okay, got it. Is e = Cv T correct?
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   April 17, 2020, 14:32
Default
  #66
New Member
 
saeedbd
Join Date: Feb 2015
Posts: 6
Rep Power: 11
saeedbd is on a distinguished road
Yes with the considered EoSs.
I found an issue with the defined tolerance for et. So now it is being solved and this problem "I don't know why et in the new energy equation remains constant" is solved.
Tobi likes this.
saeedbd is offline   Reply With Quote

Old   April 29, 2020, 04:26
Post
  #67
New Member
 
Zhongqi Zuo
Join Date: May 2018
Location: China
Posts: 8
Rep Power: 8
MrZZQi is on a distinguished road
Hi openFoamers,

Thanks for your great discussion, it really helps a lot.

However, when I look through the code, I find this term very confusing to me

Code:
p_rghEqnComp1 & p_rgh
This term is explained as 'p_rgh in p_rghEqnComp1' by Richard, and treated as 'Dp/Dt', so did Daniel do in his derivation.

But as I know & is "inner product", the operator is redefined in fvMatrix.C. p_rghEqnComp1 is a fvMatrix, p_rgh is a scalar field, how can the term be interpreted as Dp/Dt?

Anybody can help? Thanks a lot.

Zuo
MrZZQi is offline   Reply With Quote

Old   September 9, 2021, 15:36
Default
  #68
Member
 
Join Date: Feb 2020
Posts: 90
Rep Power: 6
Shibi is on a distinguished road
Hello to all,

I am also trying to understand the formulation of compressibleInterFoam for OpenFOAM ESI. However, the formulation is not clear to me.

I would like to request a further clarification on the formulation of compressibleInterFoam.

From the paper of Miller et al [1], previously referred to in this post, the pressure equation should be:

\left ( \frac{\alpha_1 \psi_1}{\rho1}+\frac{\alpha_2 \psi_2}{\rho2} \right )\left [ \frac{\partial P}{\partial t} + \vec{v} \cdot \nabla P\right ] + \nabla \cdot \vec{v}=0

Or, to better use the divergence theorem:

\left ( \frac{\alpha_1 \psi_1}{\rho1}+\frac{\alpha_2 \psi_2}{\rho2} \right )\left [ \frac{\partial p}{\partial t} + \nabla \cdot \left ( p \vec{v} \right) - p \left ( \nabla \cdot \vec{v} \right)  \right] + \nabla \cdot \vec{v}=0

With the last term on the lefh hand side, \nabla \cdot \vec{v}, we create a incompressiblePEqn and with the remainder terms a compressiblePEqn.

I took a look into the compressibleInterFoam from foam-exted. The pEqn.H has:

An incomplete CompressiblePEqn written as:
Code:
    if (pimple.transonic())
    {
        pEqnComp =
            (fvm::ddt(p) + fvm::div(phi, p) - fvm::Sp(fvc::div(phi), p));
    }
    else
    {
        pEqnComp =
            (fvm::ddt(p) + fvc::div(phi, p) - fvc::Sp(fvc::div(phi), p));
    }
Which should be: \left [ \frac{\partial p}{\partial t} + \nabla \cdot \left ( p \vec{v} \right) - p \left ( \nabla \cdot \vec{v} \right) \right]

The incompressiblePEqn which is derived by substituting the cell center velocity from the momentum equation.

Code:
        fvScalarMatrix pEqnIncomp
        (
            fvc::div(phi)
          - fvm::laplacian(rUAf, p)
        );
Now, the complete pressure Equation is assembled and solved as:

Code:
        solve
        (
            (
                max(alpha1, scalar(0))*(psi1/rho1)
              + max(alpha2, scalar(0))*(psi2/rho2)
            )
           *pEqnComp()
          + pEqnIncomp
        );
\left ( \frac{\alpha_1 \psi_1}{\rho1}+\frac{\alpha_2 \psi_2}{\rho2}  \right )\left [ \frac{\partial p}{\partial t} + \nabla \cdot \left ( p  \vec{v} \right) - p \left ( \nabla \cdot \vec{v} \right)  \right] +  \nabla \cdot \vec{v}=0

After solving the pressure equation, a dgdt term is updated with:
Code:
            dgdt =
                (pos(alpha2)*(psi2/rho2) - pos(alpha1)*(psi1/rho1))
                *(pEqnComp & p);
The volume fraction equation in [1] is written as:

\frac{\partial \alpha_1}{\partial t} + \nabla \cdot \left ( \alpha_1 \vec{v} \right) - \alpha_1 \left ( \nabla \cdot \vec{v} \right) = \alpha_1 \alpha_2\left ( \frac{\psi_1\rho_2 - \psi_2 \rho_1}{\alpha_1 \psi_1 \rho_2 + \alpha_2 \psi_2 \rho_1} \right ) \nabla \cdot \vec{v}

Here are my questions:


1º Is the formulation used in [1], the one in compressibleInterFoam?

2º Is it the same formulation on all branches of OpenFOAM (ESI, ORG and extend)?

3º is dtdg = right and side of the above equation?

4º What is the purpose of doing the dot product (&) between a scalarMatrix and a volScalarField? What is the mathematical representation of this operation?

5º In OpenFOAM(ESI) the compressible part (non-transonic) of the pressure equation we have:

Code:
        p_rghEqnComp1 =
            pos(alpha1)
           *(
                (
                    fvc::ddt(alpha1, rho1) + fvc::div(alphaPhi1*rho1f)
                  - (fvOptions(alpha1, mixture.thermo1().rho())&rho1)
                )/rho1
              - fvc::ddt(alpha1) - fvc::div(alphaPhi1)
              + (alpha1*psi1/rho1)*correction(fvm::ddt(p_rgh))
             );
Could anyone explain the lines:
Code:
                    fvc::ddt(alpha1, rho1) + fvc::div(alphaPhi1*rho1f)
                  - (fvOptions(alpha1, mixture.thermo1().rho())&rho1)
                )/rho1
               - fvc::ddt(alpha1) - fvc::div(alphaPhi1)
Additionally why is it not using the terms: \nabla \cdot \left ( p \vec{v} \right) - p \left ( \nabla \cdot \vec{v} \right) ?

6º Apart from [1] is there any other literature on the formulation of compressibleInterFoam?


Best Regards!


----
[1] -Miller, S. T., Jasak, H., Boger, D. A., Paterson, E. G., & Nedungadi, A. (2013). A pressure-based, compressible, two-phase flowa finite volume method for underwater explosions. Computers and Fluids, 87, 132–143. https://doi.org/10.1016/j.compfluid.2013.04.002
CorbinMG likes this.
Shibi is offline   Reply With Quote

Old   December 30, 2021, 01:04
Default
  #69
Member
 
hari charan
Join Date: Sep 2021
Location: India,hyderabad
Posts: 96
Rep Power: 4
saicharan662000@gmail.com is on a distinguished road
Hi Nat,
I know the post is old. But can you describe the evolution of step 4 mathematically instead of describing it in words?
Thanks in advance.
saicharan662000@gmail.com is offline   Reply With Quote

Old   December 30, 2021, 01:47
Default
  #70
Member
 
hari charan
Join Date: Sep 2021
Location: India,hyderabad
Posts: 96
Rep Power: 4
saicharan662000@gmail.com is on a distinguished road
Hello nat,
Can u explain the evolution of step 3 to step 4 using math instead of words.
Thanks in advance.
saicharan662000@gmail.com is offline   Reply With Quote

Old   January 8, 2023, 20:10
Default pEqn - what is it and how is it implemented
  #71
New Member
 
Corbin G
Join Date: Oct 2022
Location: Midwest, USA
Posts: 11
Rep Power: 3
CorbinMG is on a distinguished road
Dear FOAMers,

Thank you for all the previous contributions to this thread which have helped in my understanding of the compressibleInterFoam solver. Like several others, I am adding some inter-phase mass transfer which requires me to modify the pEqn.H and alphaEqn.H (or perhaps alphaSuSp.H). Therefore, I need a thorough understanding of their structure. I would like to document my findings here to further this thread for future FOAMers, then ask for some of your advices in areas where I am still confused.


Part 1 - interFoam
I would first like to suggest two excellent resources for understanding the PISO loop in the interFoam (incompressible two-phase volume of fluid) solver.
Deshpande et al. derive all the equations in detail, including for the PISO pressure corrector steps:
[A] Deshpande, Suraj S., Lakshman Anumolu, and Mario F. Trujillo. "Evaluating the performance of the two-phase flow solver interFoam." Computational science & discovery 5, no. 1 (2012): 014016. http://dx.doi.org/10.1088/1749-4699/5/1/014016

Next, Damian gives a line-by-line commentary of how these are implemented in the interFoam solver, including line-by-line analysis of pEqn.H. I found this very useful:
[B] Damian, S. Márquez. "Description and utilization of interFoam multiphase solver." International Center for Computational Methods in Engineering (2012): 1-64. http://www.cfdyna.com/Home/OpenFOAM/...escription.pdf



Part 2 - compressibleInterFoam introduction
I guess there are three main forks of OpenFOAM which all differ slightly. The source code for the compressibleInterFoam solver for each of these versions can be found:
foundation OpenFOAM-10: https://github.com/OpenFOAM/OpenFOAM...sibleInterFoam
ESI v2206: https://develop.openfoam.com/Develop...sibleInterFoam
foam-extended-5.0: https://sourceforge.net/p/foam-exten...ibleInterFoam/

The foam-extended version has the best documentation in the literature and I will focus on that in this post. It is isothermal (i.e. there is no TEqn.H) and therefore differs substantially from the other versions.
The ESI and foundation versions are are very similar. Both solve for temperature in TEqn.H. The foundation version seems to include some built-in functionality for inter-phase mass transfer through the fvModels options. However, the pEqn.H of these two versions is not clear to me. I plan to ask for some advices on these in a later post.


Part 3A - compressibleInterFoam foam-extended-5.0 references
There are several publications which are closely related to the foam-extended version and can fairly straightforwardly be seen in the pEqn.H. H. Jasak is a co-author on [1] which explains why it more clearly explains the foam-extended version.
These include:
[1] Miller, S. T., Hrvoje Jasak, D. A. Boger, E. G. Paterson, and A. Nedungadi. "A pressure-based, compressible, two-phase flow finite volume method for underwater explosions." Computers & Fluids 87 (2013): 132-143. http://dx.doi.org/10.1016/j.compfluid.2013.04.002
[2] Koch, Max, Christiane Lechner, Fabian Reuter, Karsten Köhler, Robert Mettin, and Werner Lauterborn. "Numerical modeling of laser generated cavitation bubbles with the finite volume and volume of fluid method, using OpenFOAM." Computers & Fluids 126 (2016): 71-90. http://dx.doi.org/10.1016/j.compfluid.2015.11.008
[3] Max Koch Master thesis: Numerical modelling of cavitation bubbles with the Finite Volume method, 2014. https://www.researchgate.net/publica..._Volume_method

Of these, [1] and [2] lay out all the essential equations while [3] provides a more detailed discussion of how they are implemented in the foam-extended code.

OK, let's go to the equations and code.


Part 3B - compressibleInterFoam foam-extended-5.0 pressure equation
The basic form of the pressure equation in Miller et al. [1] Equation 15 and Koch et al. [2] Equation 22 is:
\left(\frac{\alpha_{1}}{\rho_{1}}\Psi_{1}+\frac{\alpha_{2}}{\rho_{2}}\Psi_{2}\right)  \left( \frac{\partial p}{\partial t} + \nabla\cdot\left( 
p \vec{U} \right) - p \nabla\cdot\vec{U} \right) + \nabla\cdot\vec{U} = 0 Eq 1

Recall: \frac{D p}{D t}  = \frac{\partial p}{\partial t} + \vec{U}\cdot\nabla p  =   \frac{\partial p}{\partial t} + \nabla\cdot\left( 
p \vec{U}\right) - p \nabla\cdot\vec{U}, based on definition of material derivative and some vector identities

Now, looking into the foam-extended pEqn.H, pEqnComp is
defined below which is the second term in parenthesis in Eq 1, basically \frac{D p}{D t}.
Code:
        pEqnComp =
            (fvm::ddt(p) + fvc::div(phi, p) - fvc::Sp(fvc::div(phi), p));
Later, we get pEqnIncomp which represents the \nabla\cdot\vec{U} from Eq 1. (See one of the aforemetnioned 2012 publications [A] or [B] on how this the incompressible pressure equation is derived from substituting in a momentum expression into the incompressible continuity equation)
Code:
        fvScalarMatrix pEqnIncomp
        (
            fvc::div(phi)
          - fvm::laplacian(rUAf, p)
        );
Finally, the complete pressure equation is assembled and solved which indeed looks identical to Eq 1. Therefore I am happy and believe that foam-extended is actually solving the pressure equation from [1] and [2].
Code:
        solve
        (
            (
                max(alpha1, scalar(0))*(psi1/rho1)
              + max(alpha2, scalar(0))*(psi2/rho2)
            )
           *pEqnComp()
          + pEqnIncomp
        );

Part 3C - compressibleInterFoam foam-extended-5.0 volume of fluid equation
Let's move on to the volume of fluid (VoF) equation. The basic form of the pressure equation in Miller et al. [1] Equation 24-25 and Koch et al. [2] Equation 18 is:
\frac{\partial\alpha_{1}}{\partial t} + \nabla\cdot\left(\alpha_{1}\vec{U}\right)  + \nabla\cdot\left(\alpha_{1}\alpha_{2}\vec{U_{r}}\right) = 
\alpha_{1} \alpha_{2} \left(\frac{\Psi_{2}}{\rho_{2}} - \frac{\Psi_{1}}{\rho_{1}}\right) \frac{D p}{D t} +
\alpha_{1} \nabla\cdot\vec{U} Eq 2

Now, later on in the pEqn.H we find dgdt:
Code:
            dgdt =
                (pos(alpha2)*(psi2/rho2) - pos(alpha1)*(psi1/rho1))
               *(pEqnComp & p);
Which I interpret as below. Recall the behavior of pos(x) : if x greater zero: 1.0 else 0.0. I don't know what (pEqnComp & p) does. Maybe it plugs in the new p values into pEqnComp?
dgdt = \left( \frac{\Psi_{2}}{\rho_{2}} - \frac{\Psi_{1}}{\rho_{1}} \right) \frac{D p}{D t}

Next, in the alphaEqns.H the VoF solution is completed. Recall that (see Eq 3.15 in [3]) OpenFOAM linearizes the source terms and breaks them into two parts like S = Su + Sp*x, where x is the field being solved for. We see in in the alphaEqns.H that Sp is initialized as 0 and Su is initialized as \alpha_{1} \nabla\cdot\vec{U}. The Su and Sp are then updated based on dgdt value:
Code:
        forAll(dgdt, celli)
        {
            if (dgdt[celli] > 0.0 && alpha1[celli] > 0.0)
            {
                Sp[celli] -= dgdt[celli]*alpha1[celli];
                Su[celli] += dgdt[celli]*alpha1[celli];
            }
            else if (dgdt[celli] < 0.0 && alpha1[celli] < 1.0)
            {
                Sp[celli] += dgdt[celli]*(1.0 - alpha1[celli]);
            }
        }
Checkout Section 3.1.1 of [3] for more details on why the sign of dgdt is considered. For our purposes let's just take the else if portion and see if it makes sense:
Sp = dgdt(1 - \alpha_{1})

Plugging in the previously defined dgdt gives:
Sp = (1 - \alpha_{1}) \left( \frac{\Psi_{2}}{\rho_{2}} - \frac{\Psi_{1}}{\rho_{1}} \right) \frac{D p}{D t}

Let's now plug that into the source term equation S = Su + Sp*alpha1 and recall that alpha2 = 1 - alpha1 and we see the complete source term is:
S = \alpha_{1} \nabla\cdot\vec{U} + \alpha_{1}(1 - \alpha_{1}) \left( \frac{\Psi_{2}}{\rho_{2}} - \frac{\Psi_{1}}{\rho_{1}} \right) \frac{D p}{D t} =
\alpha_{1} \nabla\cdot\vec{U} + \alpha_{1}\alpha_{2} \left( \frac{\Psi_{2}}{\rho_{2}} - \frac{\Psi_{1}}{\rho_{1}} \right) \frac{D p}{D t}

BOOM! It's the complete RHS of the VoF equation Eq 2 from Miller et al. [1] and Koch et al. [2].

Then, the VoF equation is finally solved by passing the RHS source term to the MULES::explicitSolve which I trust considers the LHS of the VoF equation:
Code:
        MULES::explicitSolve(geometricOneField(), alpha1, phi, phiAlpha1, Sp, Su, 1, 0);

Conclusion
There you have it folks. I am confident that the foam-extended-5.0 compressibleInterFoam basically solves the pressure equation and the VoF equation described by Miller et al. [1] and Koch et al. [2].

I will discuss the foundation OpenFOAM-10 and ESI v2206 in a future post where I hope you all can help me figure out the formulation.

PS1: please point out any mistakes you see and I will try to correct them
PS2: keep FOAMing!

EDIT: the pressure-velocity coupling and PISO are well-explained in the CFD Direct book Chapter 5: https://doc.cfd.direct/notes/cfd-gen...ocity-coupling
GautCFD likes this.

Last edited by CorbinMG; January 12, 2023 at 08:44. Reason: add reference to CFD Direct book
CorbinMG is offline   Reply With Quote

Old   January 10, 2023, 17:58
Default pEqn.H - ESI and foundation version
  #72
New Member
 
Corbin G
Join Date: Oct 2022
Location: Midwest, USA
Posts: 11
Rep Power: 3
CorbinMG is on a distinguished road
EDIT: My analysis is probably not correct in this post because I think I have misinterpreted the correction() function. Please provide your insights into the correction function here: Foam::correction() function

Dear FOAMers,

I will continue my previous post, this time looking into the pEqn.H from the ESI and foundation versions, which looks quite a bit different than the foam-extended I discussed previously. I will make use of the same references.

The relevant files are:
ESI pEqn.H
ESI alphaSuSp.H
foundation pEqn.H
foundation alphaSuSp.H

The foundation and ESI versions are quite similar. As of now (ESI might be updated in the future), the main difference is that foundation version has more source term functionality through the "fvModels.source" options. Maybe inter-phase mass transfer can already be accomplished with these options in the foundation version. I will copy the code from the ESI version throughout this post.

In pEqn.H (for transonic = no) we find a compressible pressure equation for each phase.
Code:
        p_rghEqnComp1 =
            pos(alpha1)
           *(
                (
                    fvc::ddt(alpha1, rho1) + fvc::div(alphaPhi1*rho1f)
                  - (fvOptions(alpha1, mixture.thermo1().rho())&rho1)
                )/rho1
              - fvc::ddt(alpha1) - fvc::div(alphaPhi1)
              + (alpha1*psi1/rho1)*correction(fvm::ddt(p_rgh))
            );

        p_rghEqnComp2 =
            pos(alpha2)
           *(
               (
                   fvc::ddt(alpha2, rho2) + fvc::div(alphaPhi2*rho2f)
                 - (fvOptions(alpha2, mixture.thermo2().rho())&rho2)
               )/rho2
             - fvc::ddt(alpha2) - fvc::div(alphaPhi2)
             + (alpha2*psi2/rho2)*correction(fvm::ddt(p_rgh))
            );
Note, the command behavior of pos(x) : if x greater zero: 1.0 else 0.0. The pos(alpha1) makes the p_rghEqnComp1 only active when alpha1 > 0. I interpret the above code as (with an analogous equation for p_rghEqnComp2):
p_rghEqnComp1 = 
\frac{1}{\rho_{1}}
\left(  \frac{\partial\alpha_{1}\rho_{1}}{\partial t} + \nabla\cdot\left( \alpha_{1}\rho_{1}\vec{U} \right)  \right) 
- \left( \frac{\partial \alpha_{1}}{\partial t} + \nabla\cdot\left( \alpha_{1} \vec{U}\right) \right)
+ \alpha_{1}\frac{\Psi_{1}}{\rho_{1}}\frac{\partial p_{rgh}}{\partial t}

Back in the "if (pimple.transonic())" portion of pEqn.H you will find the below code where the pressure term
(the stuff inside the "correction()" command) is expanded to include the divergence terms. I guess if the user chooses "transonic no" the solver assumes the velocity is fairly low and the fvm::ddt(p_rgh) dominates the material derivative of pressure (see my previous post for expansion of Dp/Dt term). I guess in the "transonic no" selection we are assuming \frac{Dp_{rgh}}{Dt} \approx \frac{\partial p_{rgh}}{\partial t}.
Code:
        p_rghEqnComp1 =
            pos(alpha1)
           *(
                (
                    fvc::ddt(alpha1, rho1) + fvc::div(alphaPhi1*rho1f)
                  - (fvOptions(alpha1, mixture.thermo1().rho())&rho1)
                )/rho1
              - fvc::ddt(alpha1) - fvc::div(alphaPhi1)
              + (alpha1/rho1)
               *correction
                (
                    psi1*fvm::ddt(p_rgh)
                  + fvm::div(phid1, p_rgh) - fvm::Sp(fvc::div(phid1), p_rgh)
                )
            );

Next, pEqn.H defines the incompressible portion of the pressure equation as below. This is the same (less the p versus p_rgh difference) across all three version of OpenFOAM. You can checkout the Damian [B] Eq 73, Eq 76, Eq 100, and Eq 124 from my last post to understand this one. I will stick with saying this represents the \nabla\cdot U part of the pressure equation.
Code:
        fvScalarMatrix p_rghEqnIncomp
        (
            fvc::div(phiHbyA)
          - fvm::laplacian(rAUf, p_rgh)
        );
The final pressure equation is assembled and solved as:
Code:
        solve
        (
            p_rghEqnComp1() + p_rghEqnComp2() + p_rghEqnIncomp,
            mesh.solver(p_rgh.select(pimple.finalInnerIter()))
        );
Which I interpret as:
\frac{1}{\rho_{1}} \left(  \frac{\partial\alpha_{1}\rho_{1}}{\partial t} + \nabla\cdot\left( \alpha_{1}\rho_{1}\vec{U} \right)  \right) 
- \left( \frac{\partial \alpha_{1}}{\partial t} + \nabla\cdot\left( \alpha_{1} \vec{U}\right) \right)
+ \alpha_{1}\frac{\Psi_{1}}{\rho_{1}}\frac{\partial p_{rgh}}{\partial t} +
\frac{1}{\rho_{2}} \left(  \frac{\partial\alpha_{2}\rho_{2}}{\partial t} + \nabla\cdot\left( \alpha_{2}\rho_{2}\vec{U} \right)  \right) 
- \left( \frac{\partial \alpha_{2}}{\partial t} + \nabla\cdot\left( \alpha_{2} \vec{U}\right) \right)
+ \alpha_{2}\frac{\Psi_{2}}{\rho_{2}}\frac{\partial p_{rgh}}{\partial t} +
\nabla\cdot U = 0

The first term in parenthesis for p_rghEqnComp1 and p_rghEqnComp2 is just the phase mass balance equation, which should be = 0 (see refs [1] and [2]). Maybe it is included just to allow fvOption functionality for boiling, condensation, etc. when phase mass balance \neq 0. In any case, I will assume both those terms equal 0. The second term in parenthesis is the phase mass balance for incompressible (i.e. constant density) flow, like used in the interFoam solver. I am not sure why these are included. However, assuming the phase mass balance terms go to 0 simplifies the pressure equation being solved to:
- \left( \frac{\partial \alpha_{1}}{\partial t} + \nabla\cdot\left( \alpha_{1} \vec{U}\right) \right)
- \left( \frac{\partial \alpha_{2}}{\partial t} + \nabla\cdot\left( \alpha_{2} \vec{U}\right) \right)
+
\left( \alpha_{1}\frac{\Psi_{1}}{\rho_{1}} + \alpha_{2}\frac{\Psi_{2}}{\rho_{2}}\right) \frac{\partial p_{rgh}}{\partial t} 
 +  \nabla\cdot U = 0

There you have it. Less the incompressible phase mass balance terms, the pressure equation in ESI and foundation version basically looks like Miller et al. [1] and Koch et al. [2] (see Eq 1 in my previous post). Comments on the purpose of including the below in the pressure equation are welcome.
- \left( \frac{\partial \alpha_{1}}{\partial t} + \nabla\cdot\left( \alpha_{1} \vec{U}\right) \right)
- \left( \frac{\partial \alpha_{2}}{\partial t} + \nabla\cdot\left( \alpha_{2} \vec{U}\right) \right)

Towards the end of the pEqn.H, dgdt is again defined very similarly to my previous post. Then, the volume of fluid equation is setup in alphaSuSp.H and alphaEqn.H. I won't repeat the analysis here.

Note: Be aware that p_{rgh}=p-\rho \vec{g}\cdot\vec{h}

Best regards,
Corbin
arjun likes this.

Last edited by CorbinMG; January 18, 2023 at 15:19. Reason: I am probably wrong...
CorbinMG is offline   Reply With Quote

Old   June 26, 2023, 07:42
Default pEqn.H ESI version
  #73
New Member
 
Dennis Thuy
Join Date: Apr 2022
Posts: 10
Rep Power: 4
dplthuy is on a distinguished road
Hi Corbin,

Thank you for your elaborate analysis of the pressure equation! I agree with your interpretation of the equation from the ESI version. Unfortunately, I am also not able to explain what exactly the "correction()" function does.

I want to comment specifically on the two terms in the pressure equation that represent the phase mass balance for incompressible flow:
- \left( \frac{\partial \alpha_{1}}{\partial t} + \nabla\cdot\left( \alpha_{1} \vec{U}\right) \right)
- \left( \frac{\partial \alpha_{2}}{\partial t} + \nabla\cdot\left( \alpha_{2} \vec{U}\right) \right)
Since \alpha_{1} + \alpha_{2} = 1, we can write:
- \left( \frac{\partial \left( \alpha_{1} + \alpha_{2}\right)}{ \partial t} + \left( \alpha_{1} + \alpha_{2} \right) \nabla \cdot \vec{U} \right) = -\nabla \cdot \vec{U}

As compressible phase mass balance terms should be equal to zero, this additionally reduces the pressure equation to:
\left( \alpha_{1}\frac{\Psi_{1}}{\rho_{1}} + \alpha_{2}\frac{\Psi_{2}}{\rho_{2}}\right) \frac{\partial p_{rgh}}{\partial t}= 0

This formulation is significantly different from the formulation in the paper by Miller, as it no longer includes the divergence of the velocity field. Furthermore, as the terms between parenthesis are not equal to zero, except for the incompressible case, this implies that \frac{\partial p_{rgh}}{\partial t}= 0. This is clearly not the desired behavior, and also is not seen in simulation results, where p_rgh does change over time.
Am I making a mistake in rewriting the terms above, or is my observation correct? And if it is correct, what reason do we have to introduce these terms into the pressure equation?

Apart from raising additional questions, I would also like to point out that the pressure equation in the ESI version does show the expected behavior in the incompressible limit (i.e. \psi_{1} = \psi_{2} = 0 and \frac{\partial \rho_{1}}{\partial t} = \frac{\partial \rho_{2}}{\partial t} = 0 ). In that case, it reduces to the incompressible contribution, \nabla \cdot \vec{U} = 0. This, however, would also be the case if the incompressible phase mass balance terms were not included in the pressure equation.

If you have gained any additional insight in the formulation of the pressure equation in the ESI version since your last post, I would be very grateful if you could share this!

Kind regards,
Dennis
dplthuy is offline   Reply With Quote

Reply

Tags
compressible, compressibleinterfoam, theory

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Low Reynolds Number k-epsilon formulation CFX 10.0 Chris CFX 4 December 7, 2009 23:51
Immersed Boundary Formulation Rave Main CFD Forum 0 August 11, 2008 14:55
DPM Steady formulation with collisions kulwinder FLUENT 0 May 22, 2004 18:44
energy equation formulation Pedro Phoenics 1 July 5, 2001 12:17
Compressible vs. Incompressible formulations Fernando Velasco Hurtado Main CFD Forum 3 January 7, 2000 16:51


All times are GMT -4. The time now is 22:02.